NASTRAN solve failure due to E5004

[gsl58]

I am trying to run a static analysis on a school project but whenever I try to use fusion's analysis tool the simulation fails and gives this error message: 

with the suggestions:

However, I've checked my model and it seems like everything is properly constrained. In addition, the precheck tool is showing that there isn't any errors so I'm honestly confused as to what could be causing this? I've also verified that the mesh is working properly before solving so I'm pretty sure it isn't something with that.

[John_Holtz · Accepted solution]

Hi @gsl58 

For the benefit of other readers, the E5004 error (and other warnings in the image) are shown in the output file. The output file can be accessed from the browser: right-click on "Results > Solver Data > Solver Output".

The lack of stiffness is caused by three things:

1. missing constraint or contact. Based on the Check, this does not seem to be the problem.
2. bad material properties which can cause a numerical problem. For example, Poisson's ratio of 0.5 leads to a 0 somewhere in a linear static analysis. Since everything is steel, the material should be okay.
3. distorted mesh which can cause a numerical problem.

The way to test which item is the problem is to perform a Modal Frequencies analysis.

• If the analysis completes, the first frequency or frequencies will be near 0, and the piece that is moving by itself or the most is the problem.
• If the analysis fails, it is due to a distorted mesh.

It looks like there are modeling problems. The part highlighted in the image below appears to pass through other parts and either has other tubes that are inside or maybe coincidence with the highlighted tube. 

In my opinion, Fusion Simulation and creating a solid model is not the proper tool to use. Truss-like structures such as bridges should be analyzed using beam and truss elements. Inventor Nastran or Robot Structural Analysis is the proper app to use for beam/truss models. Although these structures can be modeled using solids, it takes longer to mesh, longer to solve, and is more difficult to setup the contact to duplicate the real connections. For example, you have hangers with a clevis and pin on the top end. That is not modeled accurately by using bonded contact. (It is hard to model the correct contact in solids without using separation contact, and separation contact will make the analysis run long. 3 time longer? 10 times longer? 100 times longer?) For example,  if you need to change the shape to a larger or smaller beam, you have to change the solid model and repeat. (If you use a beam model, you change the input numbers of area and moment of inertia for the new cross-section, and you have new results in a few seconds.)

Let us know if you have any other questions.

John

[jesus.rodriguezX55VX · Accepted solution]

Hello @gsl58 :   The problem that you are encountering is due to not-recommended modelling practices.  For example, the body "bolt v2:16" is modelled as a single body but contains multiple bodies:

Some bodies or lumps in Body1 of bolt v2:16 are not connected at all, making the solver fail, for example:

We strongly recommend modelling each body independently (instead of lumping them into a "single body") and then define the appropriate contact conditions.  The assembly contains several cases like the one described above.  A simple interference check in the simplify environment reveals that many bodies are interfering with each other, which is an indicator of lack of proper contact between components in the assembly, for example:  

[gsl58]

Hi John,

Thanks for taking the time to look through this! I agree that this tool is most likely not the correct one for our goals so I'll be taking a look at some of the other methods you mentioned. Again thanks for your help with this and the feedback you provided,

-Gabriel